Problem with post processor

[Anonymous]

I am using an old NUM750 cnc controller, and I am having sometimes problems with G02 and G03 commands.

This controller does not understand if both x and y values are not present after G02 or G03.

I am using post processor NUM. How can I force it to write always both X and Y values, even if one does not change from previous command?

[Tomek.G · Accepted solution]

Hi @Anonymous,

You can simple add an forcing routine at the beginig of the onCircular() function like below

function onCircular(clockwise, cx, cy, cz, x, y, z, feed) {
  xOutput.reset();
  yOutput.reset();
...}

[Anonymous · Accepted solution]

Great! Thank you very much! I will try it.

Question:

-Can I force also z-values in it , in case of circular interpolation in another plane by just adding 

zOutput.reset();

[Tomek.G · Accepted solution]

Hi @Anonymous,

sure you can!
Or you can use function 

forceXYZ();

to force all (XYZ) in one line.

[serge.quiblier]

Hello @Anonymous 

For your information, the NUM library post had been updated for several potential issues on circular interpolation.

(XYZ should no be modal, as IJK)

We should not generate a negative radii for arc over 180 degrees....

Have a nice day

Regards.